G Codes

JavaScript must be enabled in your browser to display the table of contents.

1. Conventions

Conventions used in this section

In the G code prototypes the hyphen (-) stands for a real value
and (<>) denotes an optional item.

If L- is written in a prototype the - will often be referred to
as the L number, and so on for any other letter.

In the G code prototypes the word axes stands for any axis as defined
in your configuration.

An optional value will be written like this <L->.

A real value may be:

An explicit number, 4

An expression, [2+2]

A parameter value, #88

A unary function value, acos[0]

In most cases, if axis words are given
(any or all of X Y Z A B C U V W),
they specify a destination point.

Axis numbers are in the currently active coordinate system,
unless explicitly described as being
in the absolute coordinate system.

Where axis words are optional, any omitted axes will retain their original value.

Any items in the G code prototypes not explicitly described as
optional are required.

The values following letters are often given as explicit numbers.
Unless stated otherwise, the explicit numbers can be real values. For
example, G10 L2 could equally well be written G[2*5] L[1+1]. If the
value of parameter 100 were 2, G10 L#100 would also mean the same.

If L- is written in a prototype the - will often be referred to
as the L number, and so on for any other letter.

3. G0 Rapid Move

G0 axes

For rapid motion, program G0 axes, where all the axis words are optional.
The G0 is optional if the current motion mode is G0. This will produce
coordinated motion to the destination point at the maximum rapid rate
(or slower). G0 is typically used as a positioning move.

3.1. Rapid Velocity Rate

The MAX_VELOCITY setting in the ini file [TRAJ] section defines the maximum
rapid traverse rate. The maximum rapid traverse rate can be higher than the
individual axes MAX_VELOCITY setting during a coordinated move. The maximum
rapid traverse rate can be slower than the MAX_VELOCITY setting in the [TRAJ]
section if an axis MAX_VELOCITY or trajectory constraints limit it.

If cutter compensation is active, the motion will differ from
the above; see the Cutter Compensation Section.

If G53 is programmed on the same line, the motion will also differ;
see the G53 Section for more information.

The path of a G0 rapid motion can be rounded at direction changes and depends
on the trajectory control settings and maximum
acceleration of the axes.

It is an error if:

An axis letter is without a real value.

An axis letter is used that is not configured

4. G1 Linear Move

G1 axes

For linear (straight line) motion at programed feed rate
(for cutting or not), program G1 'axes', where all the axis words are
optional. The G1 is optional if the current motion mode is G1. This will
produce coordinated motion to the destination point at the current feed
rate (or slower).

G1 Example

G90 (set absolute distance mode)
G1 X1.2 Y-3 F10 (linear move at a feed rate of 10 from current position to X1.2 Y-3)
Z-2.3 (linear move at same feed rate from current position to Z-2.3)
Z1 F25 (linear move at a feed rate of 25 from current position to Z1)
M2 (end program)

5. G2, G3 Arc Move

A circular or helical arc is specified using either G2 (clockwise
arc) or G3 (counterclockwise arc) at the current
feed rate. The direction (CW, CCW) is as viewed from the
positive end of the axis about which the circular motion occurs.

The axis of the circle or helix must be parallel to the
X, Y, or Z axis of the machine coordinate system.
The axis (or, equivalently, the plane perpendicular to the axis)
is selected with G17 (Z-axis, XY-plane),
G18 (Y-axis, XZ-plane), or G19 (X-axis, YZ-plane).
Planes 17.1, 18.1, and 19.1 are not currently supported.
If the arc is circular,
it lies in a plane parallel to the selected plane.

To program a helix, include the axis word perpendicular to the arc
plane: for example, if in the G17 plane, include a Z word. This
will cause the Z axis to move to the programmed value during the
circular XY motion.

To program an arc that gives more than one full turn, use the P word
specifying the number of full turns plus the programmed arc. The P word
must be an integer. If P is unspecified, the behavior is as if P1 was
given: that is, only one full or partial turn will result. For example, if a
180 degree arc is programmed with a P2, the resulting motion will be 1 1/2
rotations. For each P increment above 1 an extra full circle is added to the
programmed arc. Multi turn helical arcs are supported and give motion useful
for milling holes or threads.

If a line of code makes an arc and includes rotary axis motion,
the rotary axes turn at a constant rate so that the rotary
motion starts and finishes when the XYZ motion starts and finishes.
Lines of this sort are hardly ever programmed.

If cutter compensation is active, the motion will differ from
the above; see the Cutter Compensation Section.

The arc center is absolute or relative as set by G90.1 or G91.1 respectively.

Two formats are allowed for specifying an arc:
Center Format and Radius Format.

It is an error if:

No feed rate has been set.

The P word is not an integer.

5.1. Center Format Arcs

Center format arcs are more accurate than radius format arcs and are
the preferred format to use.

The end point of the arc along with the offset to the center of the
arc from the current location are used to program arcs that are less
than a full circle. It is OK if the end point of the arc is the same
as the current location.

The offset to the center of the arc from the current location and
optionally the number of turns are used to program full circles.

When programming arcs an error due to rounding can result from using a
precision of less than 4 decimal places (0.0000) for inch and less than
3 decimal places (0.000) for millimeters.

Incremental Arc Distance Mode

Arc center offsets are a relative distance from the start location of the arc.
Incremental Arc Distance Mode is default.

One or more axis words and one or more offsets must be programmed for an
arc that is less than 360 degrees.

No axis words and one or more offsets must be programmed for full circles.
The P word defaults to 1 and is optional.

For more information on 'Incremental Arc Distance Mode see the
G91.1 section.

Absolute Arc Distance Mode

Arc center offsets are the absolute distance from the current 0 position of the axis.

One or more axis words and both offsets must be programmed for arcs
less than 360 degrees.

No axis words and both offsets must be programmed for full circles.
The P word defaults to 1 and is optional.

For more information on 'Absolute Arc Distance Mode see the
G90.1 section.

When the arc is projected on the selected plane, the distance from
the current point to the center differs from the distance from the end
point to the center by more than (.05 inch/.5 mm)
OR ((.0005 inch/.005mm) AND .1% of radius).

Deciphering the Error message Radius to end of arc differs from radius to start:

start - the current position

center - the center position as calculated using the i, j, or k words

end - the programmed end point

r1 - radius from the start position to the center

r2 - radius from the end position to the center

5.2. Center Format Examples

Calculating arcs by hand can be difficult at times. One option is to
draw the arc with a cad program to get the coordinates and offsets.
Keep in mind the tolerance mentioned above, you may have to change the
precision of your cad program to get the desired results. Another
option is to calculate the coordinates and offset using formulas. As
you can see in the following figures a triangle can be formed from the
current position the end position and the arc center.

In the following figure you can see the start position is X0 Y0, the
end position is X1 Y1. The arc center position is at X1 Y0. This gives
us an offset from the start position of 1 in the X axis and 0 in the Y
axis. In this case only an I offset is needed.

G2 Example Line

G0X0Y0G2X1Y1I1F10 (clockwise arc in the XY plane)

Figure 1. G2 Example

In the next example we see the difference between the offsets for Y if
we are doing a G2 or a G3 move. For the G2 move the start position is
X0 Y0, for the G3 move it is X0 Y1. The arc center is at X1 Y0.5 for
both moves. The G2 move the J offset is 0.5 and the G3 move the J
offset is -0.5.

G2-G3 Example Line

G0X0Y0G2X0Y1I1J0.5F25 (clockwise arc in the XY plane)G3X0Y0I1J-0.5F25 (counterclockwise arc in the XY plane)

Figure 2. G2-G3 Example

In the next example we show how the arc can make a helix in the Z axis
by adding the Z word.

G2 Example Helix

G0X0Y0Z0G17G2X10Y16I3J4Z-1(helix arc with Z added)

In the next example we show how to make more than one turn using the P word.

P word Example

G0 X0 Y0 Z0
G2 X0 Y1 Z-1 I1 J0.5 P2 F25

In the center format, the radius of the arc is not specified, but it
may be found easily as the distance from the center of the circle to
either the current point or the end point of the arc.

5.3. Radius Format Arcs

G2 or G3 axes R- <P->

R - radius from current position

It is not good practice to program radius format arcs that are nearly
full circles or nearly semicircles because a small change in the
location of the end point will produce a much larger change in the
location of the center of the circle (and, hence, the middle of the
arc). The magnification effect is large enough that rounding error in a
number can produce out-of-tolerance cuts. For instance, a 1%
displacement of the endpoint of a 180 degree arc produced a 7%
displacement of the point 90 degrees along the arc. Nearly full circles
are even worse. Other size arcs (in the range tiny to 165 degrees or
195 to 345 degrees) are OK.

In the radius format, the coordinates of the end point of the arc in
the selected plane are specified along with the radius of the arc.
Program G2axesR- (or use G3 instead of G2 ). R is the
radius. The axis words are all optional except that at
least one of the two words for the axes in the selected plane must be
used. The R number is the radius. A positive radius indicates that the
arc turns through less than 180 degrees, while a negative radius
indicates a turn of more than 180 degrees. If the arc is helical, the
value of the end point of the arc on the coordinate axis parallel to
the axis of the helix is also specified.

It is an error if:

both of the axis words for the axes of the selected plane are omitted

the end point of the arc is the same as the current point.

G2 Example Line

G17G2X10Y15R20Z5(radius format with arc)

The above example makes a clockwise (as viewed from the positive Z-axis)
circular or helical arc whose axis is parallel to the Z-axis, ending
where X=10, Y=15, and Z=5, with a radius of 20. If the starting value
of Z is 5, this is an arc of a circle parallel to the XY-plane;
otherwise it is a helical arc.

6. G4 Dwell

G4 P-

P - seconds to dwell (floating point)

The P number is the time in seconds that all axes will remain unmoving.
The P number is a floating point number so fractions of a second may be used.
G4 does not affect spindle, coolant and any I/O.

G4 Example Line

G4 P0.5 (wait for 0.5 seconds before proceeding)

It is an error if:

the P number is negative or not specified.

7. G5 Cubic Spline

G5 X- Y- <I- J-> P- Q-

I - X incremental offset from start point to first control point

J - Y incremental offset from start point to first control point

P - X incremental offset from end point to second control point

Q - Y incremental offset from end point to second control point

G5 creates a cubic B-spline in the XY plane with the X and Y axes only.
P and Q must both be specified for every G5 command.

For the first G5 command in a series of G5 commands, I and J must both
be specified. For subsequent G5 commands, either both I and J must be
specified, or neither. If I and J are unspecified, the starting
direction of this cubic will automatically match the ending direction of
the previous cubic (as if I and J are the negation of the previous P and
Q).

For example, to program a curvy N shape:

G5 Sample initial cubic spline

G90 G17
G0 X0 Y0
G5 I0 J3 P0 Q-3 X1 Y1

A second curvy N that attaches smoothly to this one can now be made
without specifying I and J:

G5 Sample subsequent cubic spline

G5 P0 Q-3 X2 Y2

It is an error if:

P and Q are not both specified

Just one of I or J are specified

I or J are unspecified in the first of a series of G5 commands

An axis other than X or Y is specified

The active plane is not G17

8. G5.1 Quadratic Spline

G5.1 X- Y- I- J-

I - X incremental offset from start point to control point

J - Y incremental offset from start point to control point

G5.1 creates a quadratic B-spline in the XY plane with the X and Y axis
only. Not specifying I or J gives zero offset for the unspecified axis,
so one or both must be given.

For example, to program a parabola, through the origin, from X-2 Y4 to X2 Y4:

G5.1 Sample quadratic spline

G90 G17
G0 X-2 Y4
G5.1 X2 I2 J-8

It is an error if:

both I and J offset are unspecified or zero

An axis other than X or Y is specified

The active plane is not G17

9. G5.2 G5.3 NURBS Block

G5.2 <P-> <X- Y-> <L->
X- Y- <P->
...
G5.3

Warning: G5.2, G5.3 is experimental and not fully tested.

G5.2 is for opening the data block defining a NURBS and G5.3 for
closing the data block. In the lines between these two codes the curve
control points are defined with both their related weights (P) and
the parameter (L) which determines the order of the curve.

The current coordinate, before the first G5.2 command, is always taken
as the first NURBS control point. To set the weight for this first
control point, first program G5.2 P- without giving any X Y.

The default weight if P is unspecified is 1. The default order if L is
unspecified is 3.

G5.2 Example

G0X0Y0(rapid move)F10 (set feed rate)G5.2P1L3X0Y1P1X2Y2P1X2Y0P1X0Y0P2G5.3; The rapid moves show the same path without the NURBS BlockG0X0Y1X2Y2X2Y0X0Y0M2

10. G7 Lathe Diameter Mode

G7

Program G7 to enter the diameter mode for axis X on a lathe. When in
the diameter mode the X axis moves on a lathe will be 1/2 the distance
to the center of the lathe. For example X1 would move the cutter to
0.500” from the center of the lathe thus giving a 1” diameter part.

11. G8 Lathe Radius Mode

G8

Program G8 to enter the radius mode for axis X on a lathe. When in
Radius mode the X axis moves on a lathe will be the distance from the
center. Thus a cut at X1 would result in a part that is 2" in diameter.
G8 is default at power up.

12. G10 L1 Set Tool Table

G10 L1 P- axes <R- I- J- Q->

P - tool number

R - radius of tool

I - front angle (lathe)

J - back angle (lathe)

Q - orientation (lathe)

G10 L1 sets the tool table for the P tool number to the values of the words.

13. G10 L2 Set Coordinate System

G10 L2 P- <axes R->

P - coordinate system (0-9)

R - rotation about the Z axis

G10 L2 offsets the origin of the axes in the coordinate system specified to
the value of the axis word. The offset is from the machine origin established
during homing. The offset value will replace any current offsets in effect for
the coordinate system specified. Axis words not used will not be changed.

Program P0 to P9 to specify which coordinate system to change.

Table 1. Coordinate System

P Value

Coordinate System

G code

0

Active

n/a

1

1

G54

2

2

G55

3

3

G56

4

4

G57

5

5

G58

6

6

G59

7

7

G59.1

8

8

G59.2

9

9

G59.3

Optionally program R to indicate the rotation of the XY axis around the Z axis.
The direction of rotation is CCW as viewed from the positive end of the Z axis.

G10 L2 Pn does not change from the current coordinate system to the one specified by P,
you have to use G54-59.3 to select a coordinate system.

When a rotation is in effect jogging an axis will only move that axis
in a positive or negative direction and not along the rotated axis.

If a G92 origin offset was in effect before G10 L2,
it will continue to be in effect afterwards.

The coordinate system whose origin is set by a G10 command may be
active or inactive at the time the G10 is executed.
If it is currently active, the new coordinates take effect immediately.

It is an error if:

The P number does not evaluate to an integer in the range 0 to 9.

An axis is programmed that is not defined in the configuration.

G10 L2 Example Line

G10L2P1X3.5Y17.2

In the above example the origin of the first coordinate system
(the one selected by G54) is set to be X=3.5 and Y=17.2.
Because only X and Y are specified, the origin point is only moved in X and Y;
the other coordinates are not changed.

G10 L2 Example Line

G10L2P1X0Y0Z0(clear offsets for X,Y & Z axes in coordinate system 1)

The above example sets the XYZ coordinates of the coordinate system 1 to the machine origin.

14. G10 L10 Set Tool Table

G10 L10 P- axes <R- I- J- Q->

P - tool number

R - radius of tool

I - front angle (lathe)

J - back angle (lathe)

Q - orientation (lathe)

G10 L10 changes the tool table entry for tool P so that if the
tool offset is reloaded, with the machine in its current position
and with the current G5x and G92 offsets active, the current coordinates
for the given axes will become the given values. The axes that are
not specified in the G10 L10 command will not be changed. This could be
useful with a probe move as described in the G38 section.

15. G10 L11 Set Tool Table

G10 L11 P- axes <R- I- J- Q->

P - tool number

R - radius of tool

I - front angle (lathe)

J - back angle (lathe)

Q - orientation (lathe)

G10 L11 is just like G10 L10 except that instead of setting the entry
according to the current offsets, it is set so that the current
coordinates would become the given value if the new tool offset
is reloaded and the machine is placed in the G59.3 coordinate
system without any G92 offset active.

This allows the user to set the G59.3 coordinate system according to a
fixed point on the machine, and then use that fixture to measure tools
without regard to other currently-active offsets.

It is an error if:

Cutter Compensation is on

The P number is unspecified

The P number is not a valid tool number from the tool table

The P number is 0

16. G10 L20 Set Coordinate System

G10 L20 P- axes

P - coordinate system (0-9)

G10 L20 is similar to G10 L2 except that instead of setting the
offset/entry to the given value, it is set to a calculated value that
makes the current coordinates become the given value.

G10 L20 Example Line

G10 L20 P1 X1.5 (set the X axis current location in coordinate system 1 to 1.5)

It is an error if:

The P number does not evaluate to an integer in the range 0 to 9.

An axis is programmed that is not defined in the configuration.

17. G17 - G19.1 Plane Select

These codes set the current plane as follows:

G17 - XY (default)

G18 - ZX

G19 - YZ

G17.1 - UV

G18.1 - WU

G19.1 - VW

The UV, WU and VW planes do not support arcs.

It is a good idea to include a plane selection in the preamble
of each G code file.

The effects of having a plane selected are discussed in Section
G2 G3 Arcs and Section G81 G89

18. G20, G21 Units

G20 - to use inches for length units.

G21 - to use millimeters for length units.

It is a good idea to include units in the preamble
of each G code file.

19. G28, G28.1 Go/Set Predefined Position

Warning

Only use G28 when your machine is homed to a repeatable position and the
desired G28 position has been stored with G28.1.

G28 uses the values stored in parameters
5161-5166 as the X Y Z A B C U V W final point to move to. The parameter
values are absolute machine coordinates in the native machine units as
specified in the ini file. All axes defined in the ini file will be moved when
a G28 is issued. If no positions are stored with G28.1 then all axes will go to
the machine origin.

G28 - makes a rapid move from the current
position to the absolute position of the values in parameters 5161-5166.

G28 axes - makes a rapid move to the position specified by
axes including any offsets, then will make a rapid move to the absolute
position of the values in parameters 5161-5166 for all axes specified. Any
axis not specified will not move.

G28.1 - stores the current absolute position into parameters 5161-5166.

G28 Example Line

G28 Z2.5 (rapid to Z2.5 then to Z location specified in #5163)

It is an error if :

Cutter Compensation is turned on

20. G30, G30.1 Go/Set Predefined Position

Warning

Only use G30 when your machine is homed to a repeatable position and the
desired G30 position has been stored with G30.1.

G30 functions the same as G28 but uses the values stored in
parameters 5181-5186 as the X Y Z A B C U V W
final point to move to. The parameter values are absolute machine
coordinates in the native machine units as specified in the ini file.
All axes defined in the ini file will be moved when a G30 is issued. If no
positions are stored with G30.1 then all axes will go to the
machine origin.

Note

G30 parameters will be used to move the tool when a M6 is programmed
if TOOL_CHANGE_AT_G30=1 is in the [EMCIO] section of the ini file.

G30 - makes a rapid move from the current
position to the absolute position of the values in parameters 5181-5186.

G30 axes - makes a rapid move to the position specified
by axes including any offsets, then will make a rapid move to the
absolute position of the values in parameters 5181-5186 for all axes
specified. Any axis not specified will not move.

G30.1 - stores the current absolute position into parameters 5181-5186.

G30 Example Line

G30 Z2.5 (rapid to Z2.5 then to the Z location specified in #5i83)

It is an error if :

Cutter Compensation is turned on

21. G33 Spindle Synchronized Motion

G33 X- Y- Z- K-

K - distance per revolution

For spindle-synchronized motion in one direction, code G33 X- Y- Z- K-
where K gives the distance moved in XYZ for each revolution of the spindle.
For instance, if starting at Z=0, G33 Z-1 K.0625 produces
a 1 inch motion in Z over 16 revolutions of the spindle.
This command might be part of a program to produce a 16TPI thread.
Another example in metric, G33 Z-15 K1.5 produces
a movement of 15mm while the spindle rotates 10 times for a thread of 1.5mm.

Spindle-synchronized motion waits for the spindle index and spindle at speed
pins, so multiple passes line up. G33 moves end at the programmed endpoint.
G33 could be used to cut tapered threads or a fusee.

All the axis words are optional, except that at least one must be used.

Note

K follows the drive line described by X- Y- Z-. K is not parallel to
the Z axis if X or Y endpoints are used for example when cutting tapered
threads.

Technical Info

At the beginning of each G33 pass, LinuxCNC uses the spindle speed and the
machine acceleration limits to calculate how long it will take Z to
accelerate after the index pulse, and determines how many degrees the
spindle will rotate during that time. It then adds that angle to the
index position and computes the Z position using the corrected spindle
angle. That means that Z will reach the correct position just as it
finishes accelerating to the proper speed, and can immediately begin
cutting a good thread.

HAL Connections

The pins motion.spindle-at-speed and the encoder.n.phase-Z for the
spindle must be connected in your HAL file before G33 will work.
See the Integrators Manual for more information on spindle synchronized motion.

The requested linear motion exceeds machine velocity limits
due to the spindle speed

22. G33.1 Rigid Tapping

G33.1 X- Y- Z- K-

K - distance per revolution

For rigid tapping (spindle synchronized motion with return),
code G33.1 X- Y- Z- K- where K- gives the distance moved
for each revolution of the spindle.
A rigid tapping move consists of the following sequence:

Warning

If the X Y coordinates specified are not the current coordinates when
calling G33.1 for tapping the move will not be along the Z axis
but will rapid move from the current location to
the X Y location specified.

A move to the specified coordinate, synchronized with the spindle at
the given ratio and starting with a spindle index pulse.

When reaching the endpoint, a command to reverse the spindle (e.g.,
from clockwise to counterclockwise).

Continued synchronized motion beyond the specified end coordinate
until the spindle actually stops and reverses.

Continued synchronized motion back to the original coordinate.

When reaching the original coordinate,
a command to reverse the spindle a second time
(e.g., from counterclockwise to clockwise).

Continued synchronized motion beyond the original coordinate
until the spindle actually stops and reverses.

An unsynchronized move back to the original coordinate.

Spindle-synchronized motions wait for spindle index,
so multiple passes line up.
G33.1 moves end at the original coordinate.

All the axis words are optional, except that at least one must be used.

You will not be able to use a probe move until your
machine has been set up to provide a probe input signal.
The probe input signal must be connected to motion.probe-input in a .hal file.
G38.x uses motion.probe-input to determine when the probe has made (or lost) contact.
TRUE for probe contact closed (touching), FALSE for probe contact open.

Program G38.x axes to perform a straight probe operation.
The axis words are optional, except that at least one of them must be used.
The axis words together define the destination point that the probe will move towards,
starting from the current location. If the probe is not tripped before the destination
is reached G38.2 and G38.4 will signal an error.

The tool in the spindle must be a probe or contact a probe switch.

In response to this command, the machine moves the controlled point
(which should be at the center of the probe ball) in a straight line at the
current feed rate toward the programmed point.
In inverse time feed mode, the feed rate is such that the whole motion
from the current point to the programmed point would take the specified time.
The move stops (within machine acceleration limits)
when the programmed point is reached,
or when the requested change in the probe input takes place,
whichever occurs first.

After successful probing, parameters 5061 to 5069 will be set to the
coordinates of X, Y, Z, A, B, C, U, V, W of the location of the controlled point
at the time the probe changed state.
After unsuccessful probing, they are set to the coordinates of the programmed point.
Parameter 5070 is set to 1 if the probe succeeded and 0 if the probe failed.
If the probing operation failed, G38.2 and G38.4 will signal an error
by posting an message on screen if the selected GUI supports that.
And by halting program execution.

A comment of the form (PROBEOPEN filename.txt) will open
filename.txt and store the 9-number coordinate consisting of
XYZABCUVW of each successful straight probe in it.
The file must be closed with (PROBECLOSE). For more information
see the Comments Section.

An example file smartprobe.ngc is included (in the examples directory)
to demonstrate using probe moves to log to a file the coordinates of a part.
The program smartprobe.ngc could be used with ngcgui with minimal changes.

It is an error if:

the current point is the same as the programmed point.

no axis word is used

cutter compensation is enabled

the feed rate is zero

the probe is already in the target state

24. G40 Compensation Off

G40 - turn cutter compensation off. If tool compensation was on the
next move must be a linear move and longer than the tool diameter.
It is OK to turn compensation off when it is already off.

25. G41, G42 Cutter Compensation

The D word is optional; if there is no D word the radius of the currently
loaded tool will be used (if no tool is loaded and no D word is given,
a radius of 0 will be used).

If supplied, the D word is the tool number to use. This would normally
be the number of the tool in the spindle (in which case the D word is
redundant and need not be supplied), but it may be any valid tool number.

Note

G41/G42 D0 is a little special. Its behavior is different on
random tool changer machines and nonrandom tool changer machines
(see the Tool Change section). On nonrandom
tool changer machines, G41/G42 D0 applies the TLO of the tool currently
in the spindle, or a TLO of 0 if no tool is in the spindle. On random
tool changer machines, G41/G42 D0 applies the TLO of the tool T0 defined
in the tool table file (or causes an error if T0 is not defined in the
tool table).

To start cutter compensation to the left of the part profile, use G41.
G41 starts cutter compensation to the left of the programmed line
as viewed from the positive end of the axis perpendicular to the plane.

To start cutter compensation to the right of the part profile, use G42.
G42 starts cutter compensation to the right of the programmed line
as viewed from the positive end of the axis perpendicular to the plane.

The lead in move must be at least as long as the tool radius.
The lead in move can be a rapid move.

Cutter compensation may be performed if the XY-plane or XZ-plane is active.

User M100-M199 commands are allowed when Cutter Compensation is on.

The behavior of the machining center when cutter compensation
is on is described in the Cutter Compensation
Section along with code examples.

26. G41.1, G42.1 Dynamic Cutter Compensation

G41.1 & G42.1 function the same as G41 & G42 with the added scope of being able
to program the tool diameter. The L word defaults to 0 if unspecified.

It is an error if:

The YZ plane is active.

The L number is not in the range from 0 to 9 inclusive.

The L number is used when the XZ plane is not active.

Cutter compensation is commanded to turn on when it is already on.

27. G43 Tool Length Offset

G43 <H->

H - tool number (optional)

G43 enables tool length compensation. G43 changes subsequent motions
by offsetting the axis coordinates by the length of the offset. G43
does not cause any motion. The next time a compensated axis is moved,
that axis’s endpoint is the compensated location.

G43 without an H word uses the currently loaded tool from the last
Tn M6.

G43 Hn uses the offset for tool n.

Note

G43 H0 is a little special. Its behavior is different on random
tool changer machines and nonrandom tool changer machines (see the
Tool Changers section). On nonrandom tool changer
machines, G43 H0 applies the TLO of the tool currently in the spindle,
or a TLO of 0 if no tool is in the spindle. On random tool changer
machines, G43 H0 applies the TLO of the tool T0 defined in the tool
table file (or causes an error if T0 is not defined in the tool table).

G43 H- Example Line

G43 H1 (set tool offsets using the values from tool 1 in the tool table)

It is an error if:

the H number is not an integer, or

the H number is negative, or

the H number is not a valid tool number (though note that 0 is a valid
tool number on nonrandom tool changer machines, it means "the tool
currently in the spindle")

28. G43.1: Dynamic Tool Length Offset

G43.1 axes

G43.1 axes - change subsequent motions by replacing the current offset(s)
of axes. G43.1 does not cause any motion. The next time a compensated axis
is moved, that axis’s endpoint is the compensated location.

You can sum together an arbitrary number of offsets by calling G43.2
more times. There are no built-in assumptions about which numbers are geometry
offsets and which are wear offsets, or that you should have only one of each.

Like the other G43 commands, G43.2 does not cause any motion. The next time a
compensated axis is moved, that axis’s endpoint is the compensated location.

It is an error if:

H is unspecified, or

the given tool number does not exist in the tool table

Note

G43.2 does not write to the tool table.

30. G49: Cancel Tool Length Compensation

G49 - cancels tool length compensation

It is OK to program using the same offset already in use. It is also
OK to program using no tool length offset if none is currently being
used.

31. G53 Move in Machine Coordinates

G53 axes

To move in the machine coordinate system,
program G53 on the same line as a linear move. G53 is not modal and must be
programmed on each line. G0 or G1 does not have to be programmed on the same
line if one is currently active.

For example G53 G0 X0 Y0 Z0 will move the axes to the home position even if
the currently selected coordinate system has offsets in effect.

33. G61, G61.1 Exact Path Mode

G61 - Exact path mode, movement exactly as programed. Moves will slow or
stop as needed to reach every programed point. If two sequential moves are
exactly co-linear movement will not stop.

G61.1 - Exact stop mode, movement will stop at the end of each programed
segment.

34. G64 Path Blending

G64 <P- <Q->>

P - motion blending tolerance

Q - naive cam tolerance

G64 - best possible speed.

G64 P- <Q- > blending with tolerance.

G64 - without P means to keep the best speed possible, no matter how
far away from the programmed point you end up.

G64 P- Q- - is a way to fine tune your system for best compromise
between speed and accuracy. The P- tolerance means that the actual path
will be no more than P- away from the programmed endpoint. The velocity
will be reduced if needed to maintain the path. In addition, when you
activate G64 P- Q- it turns on the naive cam detector; when there are
a series of linear XYZ feed moves at the same feed rate
that are less than Q- away from being collinear, they are collapsed into a
single linear move. On G2/G3 moves in the G17 (XY) plane when the maximum
deviation of an arc from a straight line is less than the G64 P-
tolerance the arc is broken into two lines (from start of arc to
midpoint, and from midpoint to end). those lines are then subject to
the naive cam algorithm for lines. Thus, line-arc, arc-arc, and
arc-line cases as well as line-line benefit from the naive cam
detector. This improves contouring performance by simplifying the
path. It is OK to program for the mode that is already active. See also
the Trajectory Control Section for more
information on these modes.
If Q is not specified then it will have the same behavior as before and
use the value of P-.

G64 P- Example Line

G64 P0.015 (set path following to be within 0.015 of the actual path)

It is a good idea to include a path control specification in the preamble
of each G code file.

35. G73 Drilling Cycle with Chip Breaking

G73 X- Y- Z- R- Q- <L->

R - retract position along the Z axis.

Q - delta increment along the Z axis.

L - repeat

The G73 cycle is drilling or milling with chip breaking.
This cycle takes a Q number which represents a delta increment along the Z axis.

Preliminary motion.

If the current Z position is below the R position, The Z axis does a
rapid move to the R position.

Move to the X Y coordinates

Move the Z-axis only at the current feed rate downward
by delta or to the Z position, whichever is less deep.

Rapid up a bit.

Repeat steps 2 and 3 until the Z position is reached at step 2.

The Z axis does a rapid move to the R position.

It is an error if:

the Q number is negative or zero.

the R number is not specified

36. G76 Threading Cycle

G76 P- Z- I- J- R- K- Q- H- E- L-

Figure 3. G76 Threading

Drive Line - A line through the initial X position parallel to the Z.

P- - The thread pitch in distance per revolution.

Z- - The final position of threads. At the end of the cycle the tool will
be at this Z position.

Note

When G7 Lathe Diameter Mode is in force the values for I, J and K are
diameter measurements. When G8 Lathe Radius Mode is in force the values for
I, J and K are radius measurements.

I- - The thread peak offset from the drive line. Negative I values
are external threads, and positive I values are internal threads.
Generally the material has been turned to this size before the G76 cycle.

J- - A positive value specifying the initial cut depth. The first
threading cut will be J beyond the thread peak position.

K- - A positive value specifying the full thread depth. The final
threading cut will be K beyond the thread peak position.

Q- - The compound slide angle is the angle (in degrees) describing to
what extent successive passes should be offset along the drive line.
This is used to cause one side of the tool to remove more material than
the other. A positive Q value causes the leading edge of the tool to
cut more heavily.
Typical values are 29, 29.5 or 30.

H- - The number of spring passes. Spring passes are additional passes at
full thread depth. If no additional passes are desired, program H0.

E- - Specifies the distance along the drive line used for the taper. The
angle of the taper will be so the last pass tapers to the thread crest
over the distance specified with E.' E0.2' will give a taper for the
first/last 0.2 length units along the
thread. For a 45 degree taper program E the same as K

L- - Specifies which ends of the thread get the taper. Program L0 for no
taper (the default), L1 for entry taper, L2 for exit taper, or L3
for both entry and exit tapers. Entry tapers will pause at the drive line to
synchronize with the index pulse then move at the feed rate
in to the beginning of the taper. No entry taper and the tool will rapid to the
cut depth then synchronize and begin the cut.

The tool is moved to the initial X and Z positions prior to issuing
the G76. The X position is the drive line and the Z position is the
start of the threads.

The tool will pause briefly for synchronization before each threading
pass, so a relief groove will be required at the entry unless the
beginning of the thread is past the end of the material or an entry
taper is used.

Unless using an exit taper, the exit move is not synchronized to the spindle
speed and will be a rapid move. With a slow spindle, the
exit move might take only a small fraction of a revolution. If the spindle
speed is increased after several passes are complete, subsequent exit
moves will require a larger portion of a revolution, resulting in a
very heavy cut during the exit move. This can be avoided by providing a
relief groove at the exit, or by not changing the spindle speed while
threading.

The final position of the tool will be at the end of the drive line.
A safe Z move will be needed with an internal thread to remove the tool
from the hole.

It is an error if:

The active plane is not the ZX plane

Other axis words, such as X- or Y-, are specified

The R- degression value is less than 1.0.

All the required words are not specified

P-, J-, K- or H- is negative

E- is greater than half the drive line length

HAL Connections

The pins motion.spindle-at-speed and the encoder.n.phase-Z for the
spindle must be connected in your HAL file before G76 will work.
See the spindle pins in the Motion section for more
information.

Technical Info

The G76 canned cycle is based on the G33 Spindle Synchronized Motion. For more
information see the G33 Technical Info.

The sample program g76.ngc shows the use of the G76 canned cycle,
and can be previewed and
executed on any machine using the sim/lathe.ini configuration.

G76 Example

G0Z-0.5X0.2G76P0.05Z-1I-.075J0.008K0.045Q29.5L2 E0.045

In the figure the tool is in the final position after the G76 cycle
is completed. You can see the entry path on the right from the Q29.5
and the exit path on the left from the L2 E0.045. The white lines
are the cutting moves.

Figure 4. G76 Example

37. Canned Cycles

The canned cycles G81 through G89 and the canned cycle stop G80
are described in this section.

All canned cycles are performed with respect to the currently-selected
plane. Any of the nine planes may be selected. Throughout this section,
most of the descriptions assume the XY-plane has been selected. The
behavior is analogous if another plane is selected, and the correct
words must be used. For instance, in the G17.1 plane, the action of
the canned cycle is along W, and the locations
or increments are given with U and V. In this case substitute U,V,W for
X,Y,Z in the instructions below.

Rotary axis words are not allowed in canned cycles. When the
active plane is one of the XYZ family, the UVW axis words are not
allowed. Likewise, when the active plane is one of the UVW family, the
XYZ axis words are not allowed.

37.1. Common Words

All canned cycles use X, Y, Z, or U, V, W groups depending on the
plane selected and R words. The R (usually meaning retract) position is
along the axis perpendicular to the currently selected plane (Z-axis
for XY-plane, etc.) Some canned cycles use additional arguments.

37.2. Sticky Words

For canned cycles, we will call a number sticky if, when the same
cycle is used on several lines of code in a row, the number must be
used the first time, but is optional on the rest of the lines. Sticky
numbers keep their value on the rest of the lines if they are not
explicitly programmed to be different. The R number is always sticky.

In incremental distance mode X, Y, and R numbers are treated as
increments from the current position and Z as an increment from the
Z-axis position before the move involving Z takes place. In absolute
distance mode, the X, Y, R, and Z numbers are absolute positions in the
current coordinate system.

37.3. Repeat Cycle

The L number is optional and represents the number of repeats.
L=0 is not allowed. If the repeat feature is used, it is
normally used in incremental distance mode, so that the same sequence
of motions is repeated in several equally spaced places along a
straight line. When L- is greater than 1 in incremental mode with the
XY-plane selected, the X and Y positions are determined by adding the
given X and Y numbers either to the current X and Y positions (on the
first go-around) or to the X and Y positions at the end of the previous
go-around (on the repetitions). Thus, if you program L10 , you will
get 10 cycles. The first cycle will be distance X,Y from
the original location. The R and Z positions do not change during the
repeats. The L number is not sticky. In absolute distance mode,
L>1 means do the same cycle in the same place several
times, Omitting the L word is equivalent to specifying L=1.

37.4. Retract Mode

The height of the retract move at the end of each repeat (called
clear Z in the descriptions below) is determined by the setting of
the retract mode: either to the original Z position (if that is above
the R position and the retract mode is G98, OLD_Z), or otherwise to
the R position. See the G98 G99 Section.

37.5. Canned Cycle Errors

It is an error if:

axis words are all missing during a canned cycle,

axis words from different groups (XYZ) (UVW) are used together,

a P number is required and a negative P number is used,

an L number is used that does not evaluate to a positive integer,

rotary axis motion is used during a canned cycle,

inverse time feed rate is active during a canned cycle,

or cutter compensation is active during a canned cycle.

If the XY plane is active, the Z number is sticky, and it is an error
if:

the Z number is missing and the same canned cycle was not already
active,

or the R number is less than the Z number.

If other planes are active, the error conditions are analogous to the
XY conditions above.

37.6. Preliminary and In-Between Motion

Preliminary motion is a set of motions that is common to all of the
milling canned cycles. If the current Z position is below the R position,
the Z axis does a rapid move to the R position. This happens only
once, regardless of the value of L.

In addition, at the beginning of the first cycle and each repeat, the
following one or two moves are made

The Z-axis make a rapid move to the R position, if it is
not already at the R position.

If another plane is active, the preliminary and in-between motions are
analogous.

37.7. Why use a canned cycle?

There are at least two reasons for using canned cycles. The first is
the economy of code. A single bore would take several lines of code to
execute.

The G81 Example 1 demonstrates how a canned cycle could be
used to produce 8 holes with ten lines of G code within the canned cycle mode.
The program below will produce the same set of 8 holes using five lines
for the canned cycle. It does not follow exactly the same path nor does
it drill in the same order as the earlier example. But the program
writing economy of a good canned cycle should be obvious.

The G98 to the second line above means that the return move will be to
the value of Z in the first line since it is higher that the R value
specified.

Twelve Holes in a Square

This example demonstrates the use of the L word to repeat a set of
incremental drill cycles for successive blocks of code within the same
G81 motion mode. Here we produce 12 holes using five lines of code in
the canned motion mode.

The advantage of the first set is that, the G80 line clearly turns off the
G81 canned cycle. With the first set of blocks, the programmer must turn
motion back on with G0, as is done in the next line, or any other motion
mode G word.

If a canned cycle is not turned off with G80 or another motion word, the
canned cycle will attempt to repeat itself using the next block of code
that contains an X, Y, or Z word. The following file drills (G81) a set
of eight holes as shown in the following caption.

Notice the z position change after the first four holes.
Also, this is one of the few places where line numbers have some value,
being able to point a reader to a specific line of code.

Figure 5. G80 Cycle

The use of G80 in line N200 is optional because the G0 on the next
line will turn off the G81 cycle. But using the G80 as shown in
Example 1, will provide for easier to read canned cycle. Without it, it
is not so obvious that all of the blocks between N120 and N200 belong
to the canned cycle.

Suppose the current position is (X1, Y2, Z3) and the following line of NC
code is interpreted.

G91G98G81X4Y5Z-0.6R1.8L3

This calls for incremental distance mode (G91) and OLD_Z retract mode
(G98). It also calls for the G81 drilling cycle to be repeated three
times. The X value is 4, the Y value is 5, the Z value is -0.6 and the
R value is 1.8. The initial X position is 5 (=1+4), the initial Y
position is 7 (=2+5), the clear Z position is 4.8 (=1.8+3), and the Z
position is 4.2 (=4.8-0.6). OLD_Z is 3.

The first preliminary move is a maximum rapid move along the Z axis to
(X1,Y2,Z4.8), since OLD_Z < clear Z.

Now suppose that you execute the first G81 block of code but from (X0,
Y0, Z0) rather than from (X1, Y2, Z3).

G90 G98 G81 X4 Y5 Z1.5 R2.8

Since OLD_Z is below the R value, it adds
nothing for the motion but since the initial value of Z is less than
the value specified in R, there will be an initial Z move during the
preliminary moves.

Example 4 - Absolute G81 R > Z

This is a plot of the path of motion for the second g81 block of code.

G91 G98 G81 X4 Y5 Z-0.6 R1.8 L3

Since this plot starts with (X0, Y0, Z0), the interpreter adds the
initial Z0 and R1.8 and rapid moves to that location. After that initial Z
move, the repeat feature works the same as it did in example 3 with the
final Z depth being 0.6 below the R value.

Example 5 - Relative position R > Z

G90 G98 G81 X4 Y5 Z-0.6 R1.8

Since this plot starts with (X0, Y0, Z0), the interpreter adds the initial Z0
and R1.8 and rapid moves to that location as in Example 4. After that initial Z
move, the rapid move to X4 Y5 is done. Then the final Z
depth being 0.6 below the R value. The repeat function would make the Z move
in the same location again.

40. G82 Drilling Cycle, Dwell

G82 (X- Y- Z-) or (U- V- W-) R- L- P-

The G82 cycle is intended for drilling with a dwell at the bottom of
the hole.

The motion of a G82 canned cycle looks just like G81 with the
addition of a dwell at the bottom of the Z move. The length of
the dwell is specified by a P- word in the G82 block.

41. G83 Peck Drilling Cycle

G83 (X- Y- Z-) or (U- V- W-) R- L- Q-

The G83 cycle (often called peck drilling) is intended for deep
drilling or
milling with chip breaking. The retracts in this cycle clear the hole
of chips and cut off any long stringers (which are common when drilling
in aluminum). This cycle takes a Q number which represents a delta
increment along the Z-axis. The retract before final depth will always
be to the retract plane even if G98 is in effect. The final retract will
honor the G98/99 in effect. G83 functions the same as G81 with the addition
of retracts during the drilling operation.

50. G92 Coordinate System Offset

G92 axes

G92 makes the current point have the coordinates you want (without
motion), where the axis words contain the axis numbers you want.
All axis words are optional, except that at least one must be used.
If an axis word is not used for a given axis, the coordinate on
that axis of the current point is not changed.

When G92 is executed, the origins of all coordinate systems move.
They move such that the value of the current controlled point, in the currently
active coordinate system, becomes the specified value. All coordinate
system’s origins are offset this same distance.

For example, suppose the current point is at X=4 and there is
currently no G92 offset active. Then G92 x7 is programmed. This
moves all origins -3 in X, which causes the
current point to become X=7. This -3 is saved in parameter 5211.

Being in incremental distance mode has no effect on the action of G92.

G92 offsets may be already be in effect when the G92 is called.
If this is the case, the offset is replaced with a new
offset that makes the current point become the specified value.

It is an error if:

all axis words are omitted.

LinuxCNC stores the G92 offsets and reuses them on the next run of a
program. To prevent this, one can program a G92.1 (to erase them), or
program a G92.2 (to remove them - they are still stored).

51. G92.1, G92.2 Reset G92 Offsets

G92.1 only clears G92 offsets, to change G53-G59.3 coordinate system offsets
in G code use either G10 L2 or G10 L20.

52. G92.3 Restore G92 Offsets

G92.3 - set the G92 offset to the values saved in parameters 5211 to 5219

You can set axis offsets in one program and use the same offsets in
another program. Program G92 in the first program. This will set
parameters 5211 to 5219. Do not use G92.1 in the remainder of the
first program. The parameter values will be saved when the first
program exits and restored when the second one starts up.
Use G92.3 near the beginning of the second program. That will restore
the offsets saved in the first program.

53. G93, G94, G95: Feed Rate Mode

G93 - is Inverse Time Mode. In inverse time feed rate mode, an F word
means the move should be completed in [one divided by the F number]
minutes. For example, if the F number is 2.0, the move should be
completed in half a minute.

When the inverse time feed rate mode is active, an F word must appear
on every line which has a G1, G2, or G3 motion, and an F word on a line
that does not have G1, G2, or G3 is ignored. Being in inverse time feed
rate mode does not affect G0 (rapid move) motions.

G94 - is Units per Minute Mode.
In units per minute feed mode, an F word is interpreted to mean
the controlled point should move at a certain number of inches per
minute, millimeters per minute, or degrees per minute, depending upon
what length units are being used and which axis or axes are moving.

G95 - is Units per Revolution Mode
In units per revolution mode, an F word is interpreted to mean the
controlled point should move a certain number of inches per revolution
of the spindle, depending on what length units are being used and which
axis or axes are moving. G95 is not suitable for threading, for
threading use G33 or G76.
G95 requires that motion.spindle-speed-in to be connected.

It is an error if:

Inverse time feed mode is active and a line with G1, G2, or G3
(explicitly or implicitly) does not have an F word.

A new feed rate is not specified after switching to G94 or G95

54. G96, G97 Spindle Control Mode

G96 <D-> S- (Constant Surface Speed Mode)
G97 (RPM Mode)

D - maximum spindle RPM

S - surface speed

G96 D- S- - selects constant surface speed of S feet per minute
(if G20 is in effect) or meters per minute
(if G21 is in effect). D- is optional.

When using G96, ensure that X0 in
the current coordinate system (including offsets and tool lengths) is
the center of rotation or LinuxCNC will not give the desired spindle speed.
G96 is not affected by radius or diameter mode.

G97 selects RPM mode.

G96 Example Line

G96 D2500 S250 (set CSS with a max rpm of 2500 and a surface speed of 250)

It is an error if:

S is not specified with G96

A feed move is specified in G96 mode while the spindle is not turning

55. G98, G99 Canned Cycle Return Level

G98 - retract to the position that axis was in just before this series
of one or more contiguous canned cycles was started.

G99 - retract to the position specified by the R word of the canned cycle.

Program a G98 and the canned cycle will use the Z position prior to
the canned cycle as the Z return position if it is higher than the R
value specified in the cycle. If it is lower, the R value will be
used. The R word has different meanings in absolute distance mode and
incremental distance mode.

G98 Retract to Origin

G0 X1 Y2 Z3
G90 G98 G81 X4 Y5 Z-0.6 R1.8 F10

The G98 to the second line above means that the return move will be to
the value of Z in the first line since it is higher that the R value
specified.

The initial (G98) plane is reset any time cycle motion mode is
abandoned, whether explicitly (G80) or implicitly (any motion code
that is not a cycle). Switching among cycle modes (say G81
to G83) does NOT reset the initial plane. It is possible to switch
between G98 and G99 during a series of cycles.